Mitsubishi Electric EZ Motion E60/E68 Series Programming Manual

EZMotion and MELDAS are registered trademarks of Mitsubishi Electric Corporation.

Other company and product names that appear in this manual are trademarks or registered

trademarks of the respective companies.

Introduction

This manual is a guide for using the EZMotion-NC E60/E68.

Programming is described in this manual, so read this manual thoroughly before starting

programming. Thoroughly study the "Precautions for Safety" on the following page to

ensure safe use of the NC unit.

Details described in this manual

CAUTION

For items described in "Restrictions" or "Usable State", the instruction manual issued by the

machine tool builder takes precedence over this manual.

An effort has been made to note as many special handling methods in this user's manual. Items

not described in this manual must be interpreted as "not possible".

This manual has been written on the assumption that all option functions are added.

Refer to the specifications issued by the machine tool builder before starting use.

Refer to the Instruction Manual issued by each machine tool builder for details on each machine

tool.

Some screens and functions may differ depending on the NC system or its version, and some

functions may not be possible. Please confirm the specifications before use.

General precautions

(1) Refer to the following documents for details on handling

Operation Manual ........ IB-1500172

Precautions for Safety

Always read the specifications issued by the machine tool builder, this manual, related

manuals and attached documents before installation, operation, programming, maintenance

or inspection to ensure correct use.

Understand this numerical controller, safety items and cautions before using the unit.

This manual ranks the safety precautions into "DANGER", "WARNING" and "CAUTION".

When the user may be subject to imminent fatalities or major injuries if

handling is mistaken.

When the user may be subject to fatalities or major injuries if handling is

mistaken.

When the user may be subject to injuries or when physical damage may

occur if handling is mistaken.

Note that even items ranked as " CAUTION", may lead to major results depending on the

situation. In any case, important information that must always be observed is described.

DANGER

Not applicable in this manual.

WARNING

Not applicable in this manual.

CAUTION

1. Items related to product and manual

For items described as "Restrictions" or "Usable State" in this manual, the instruction manual

issued by the machine tool builder takes precedence over this manual.

An effort has been made to describe special handling of this machine, but items that are

not described must be interpreted as "not possible".

This manual is written on the assumption that all option functions are added. Refer to the

specifications issued by the machine tool builder before starting use.

Refer to the Instruction Manual issued by each machine tool builder for details on each

machine tool.

Some screens and functions may differ depending on the NC system or its version, and

some functions may not be possible. Please confirm the specifications before use.

2. Items related to operation

Before starting actual machining, always carry out dry operation to confirm the machining

program, tool offset amount and workpiece offset amount, etc.

If the workpiece coordinate system offset amount is changed during single block stop, the

new setting will be valid from the next block.

(Continued on next page)

DANGER

WARNING

CAUTION

Turn the mirror image ON and OFF at the mirror image center.

If the tool offset amount is changed during automatic operation (including during single

block stop), it will be validated from the next block or blocks onwards.

Do not make the synchronous spindle rotation command OFF with one workpiece chucked by the

basic spindle and synchronous spindle during the spindle synchronous control mode.

Failure to observe this may cause the synchronous spindle stop, and hazardous situation.

3. Items related to programming

The commands with "no value after G" will be handled as "G00".

" ; ", "EOB", "%", and "EOR" are symbols used for explanation. The actual codes for ISO are "CR,

LF" ("LF") and "%".

The programs created on the Edit screen are stored in the NC memory in a "CR, LF" format,

however, the programs created with external devices such as the FLD or RS-232C may be stored in

an "LF" format.

The actual codes for EIA are "EOB (End of Block)" and "EOR (End of Record)".

When creating the machining program, select the appropriate machining conditions, and

make sure that the performance, capacity and limits of the machine and NC are not

exceeded. The examples do not consider the machining conditions.

Do not change fixed cycle programs without the prior approval of the machine tool builder.

Contents

1. Control Axes .................................................................................................................................1

1.1 Coordinate word and control axis ...........................................................................................1

1.2 Coordinate systems and coordinate zero point symbols ........................................................2

2. Input Command Units ..................................................................................................................3

2.1 Input command units...............................................................................................................3

2.2 Input setting units....................................................................................................................3

3. Data Formats.................................................................................................................................4

3.1 Tape codes.............................................................................................................................4

3.2 Program formats.....................................................................................................................7

3.3 Program address check function ..........................................................................................10

3.4 Tape memory format.............................................................................................................11

3.5 Optional block skip ; /............................................................................................................11

3.6 Program/sequence/block numbers ; O, N.............................................................................12

3.7 Parity H/V..............................................................................................................................13

3.8 G code lists...........................................................................................................................14

3.9 Precautions before starting machining..................................................................................17

4. Buffer Register............................................................................................................................18

4.1 Input buffer............................................................................................................................18

4.2 Pre-read buffers....................................................................................................................19

5. Position Commands...................................................................................................................20

5.1 Position command methods ; G90, G91...............................................................................20

5.2 Inch/metric command change; G20, G21 .............................................................................22

5.3 Decimal point input ...............................................................................................................27

6. Interpolation Functions..............................................................................................................31

6.1 Positioning (Rapid traverse); G00.........................................................................................31

6.2 Linear interpolation; G01.......................................................................................................37

6.3 Plane selection; G17, G18, G19...........................................................................................39

6.4 Circular interpolation; G02, G03 ...........................................................................................41

6.5 R-specified circular interpolation; G02, G03.........................................................................45

6.6 Helical interpolation ; G17 to G19, G02, G03 .......................................................................47

6.7 Thread cutting.......................................................................................................................51

6.7.1 Constant lead thread cutting ; G33.................................................................................51

6.7.2 Inch thread cutting; G33 .................................................................................................55

6.8 Uni-directional positioning; G60............................................................................................56

6.9 Circular interpolation; G07.1.................................................................................................58

7. Feed Functions ...........................................................................................................................66

7.1 Rapid traverse rate ...............................................................................................................66

7.2 Cutting feed rate ...................................................................................................................66

7.3 F1-digit Feed.........................................................................................................................67

7.4 Synchronous feed; G94, G95 ...............................................................................................68

7.5 Feedrate designation and effects on control axes................................................................70

7.6 Exact stop check; G09..........................................................................................................73

7.7 Exact stop check mode ; G61...............................................................................................76

7.8 Deceleration check ...............................................................................................................76

7.8.1 G1 → G0 deceleration check..........................................................................................77

7.8.2 G1 → G1 deceleration check..........................................................................................79

7.9 Automatic corner override ; G62...........................................................................................80

7.10 Tapping mode ; G63...........................................................................................................85

7.11 Cutting mode ; G64.............................................................................................................85

8. Dwell ............................................................................................................................................86

8.1 Per-second dwell ; G04.........................................................................................................86

9. Miscellaneous Functions...........................................................................................................88

9.1 Miscellaneous functions (M8-digits BCD).............................................................................88

9.2 Secondary miscellaneous functions (B8-digits, A8 or C8-digits) ..........................................90

9.3 Index table indexing..............................................................................................................91

10. Spindle Functions.....................................................................................................................93

10.1 Spindle functions S functions..............................................................................................93

10.1.1 Spindle functions (S6-digits Analog).............................................................................93

10.1.2 Spindle functions (S8-digits).........................................................................................93

10.2 Constant surface speed control; G96, G97.........................................................................94

10.3 Spindle/C Axis Control........................................................................................................95

10.4 Spindle Synchronization Control.........................................................................................98

10.4.1 Spindle Synchronization Control II..................................................................................99

10.4.2 Precautions for Using Spindle Synchronization Control................................................104

10.5 Multiple Spindle Control....................................................................................................106

10.5.1 Multiple Spindle Control I (Multiple Spindle Command) .............................................107

10.5.2 Multiple Spindle Control I (Spindle Selection Command)...........................................108

10.5.3 Multiple Spindle Control II...........................................................................................110

11. Tool Functions........................................................................................................................112

11.1 Tool functions (T8-digit BCD)............................................................................................112

12. Tool Offset Functions.............................................................................................................113

12.1 Tool offset.........................................................................................................................113

12.2 Tool length offset/cancel; G43, G44/G49..........................................................................117

12.3 Tool radius compensation.................................................................................................120

12.3.1 Tool radius compensation operation ..........................................................................121

12.3.2 Other operations during tool radius compensation.....................................................132

12.3.3 G41/G42 commands and I, J, K designation..............................................................141

12.3.4 Interrupts during tool radius compensation ................................................................147

12.3.5 General precautions for tool radius compensation.....................................................149

12.3.6 Changing of offset No. during compensation mode....................................................150

12.3.7 Start of tool radius compensation and Z axis cut in operation....................................152

12.3.8 Interference check......................................................................................................154

12.4 Programmed offset input; G10, G11.................................................................................161

12.5 Tool position offset; G45 to G48.......................................................................................166

12.6 Inputting the tool life management data............................................................................173

13. Program Support Functions..................................................................................................176

13.1 Fixed cycles......................................................................................................................176

13.1.1 Standard fixed cycles; G80 to G89, G73, G74, G76...................................................176

13.1.2 Initial point and R point level return; G98, G99...........................................................204

13.1.3 Setting of workpiece coordinates in fixed cycle mode................................................205

13.2 Special fixed cycle; G34, G35, G36, G37.1 ......................................................................206

13.3 Subprogram control; M98, M99, M198 .............................................................................211

13.3.1 Calling subprogram with M98 and M99 commands....................................................211

13.3.2 Calling Subprogram with M198 Commands ...............................................................216

13.4 Variable commands..........................................................................................................218

13.5 User macro specifications.................................................................................................220

13.5.1 User macro commands ;G65,G66,G66.1,G67 ...........................................................220

13.5.2 Macro call instruction..................................................................................................221

13.5.3 ASCII Code Macro......................................................................................................229

13.5.4 Variables.....................................................................................................................233

13.5.5 Types of variables.......................................................................................................235

13.5.6 Arithmetic commands.................................................................................................271

13.5.7 Control commands......................................................................................................277

13.5.8 External output commands.........................................................................................280

13.5.9 Precautions.................................................................................................................282

13.5.10 Actual examples of using user macros.....................................................................284

13.6 G command mirror image; G50.1, G51.1..........................................................................288

13.7 Corner chamfering, corner rounding.................................................................................291

13.7.1 Corner chamfering " ,C_ "...........................................................................................291

13.7.2 Corner rounding " ,R_ "...............................................................................................293

13.8 Linear angle command .....................................................................................................295

13.9 Geometric command.........................................................................................................297

13.10 Polar coordinate command; G16 ....................................................................................301

13.11 Circle cutting; G12, G13..................................................................................................307

13.12 Program parameter input; G10, G11 ..............................................................................309

13.13 Macro interrupt................................................................................................................310

13.14 Tool change position return ............................................................................................319

13.15 High-accuracy control; G61.1 .........................................................................................322

13.16 High-accuracy control; G08 ............................................................................................334

13.17 High-speed machining mode..........................................................................................346

13.17.1 High-speed machining mode III................................................................................346

13.18 Scaling ; G50/G51...........................................................................................................349

13.19 Program coordinate rotation; G68/G69...........................................................................353

14. Coordinates System Setting Functions................................................................................357

14.1 Coordinate words and control axes ..................................................................................357

14.2 Basic machine, work and local coordinate systems..........................................................358

14.3 Machine zero point and 2nd, 3rd, 4th reference points (Zero point).................................359

14.4 Basic machine coordinate system ....................................................................................360

14.5 Coordinate system setting ;G92........................................................................................361

14.6 Automatic coordinate system setting................................................................................362

14.7 Reference (zero) point return; G28, G29 ..........................................................................363

14.8 2nd, 3rd and 4th reference (zero) point return; G30.........................................................367

14.9 Simple zero point return....................................................................................................370

14.10 Reference point check; G27 ...........................................................................................375

14.11 Work coordinate system setting and offset ; G54 to G59 (G54.1) ..................................376

14.12 Local coordinate system setting;.....................................................................................387

14.13 Coordinate system for rotary axis ...................................................................................391

15. Measurement Support Functions..........................................................................................394

15.1 Automatic tool length measurement; G37.........................................................................394

15.2 Skip Function; G31 ...........................................................................................................398

15.3 Multi-stage skip function; G31.n, G04...............................................................................403

15.4 Multi-skip function 2..........................................................................................................405

15.5 Programmable current limitation.......................................................................................408

Appendix 1. Program Parameter Input N No. Correspondence Table ..................................409

Appendix 2. Program Error .......................................................................................................411

Appendix 3. Order of G Function Command Priority..............................................................425

1. Control Axes

1.1 Coordinate word and control axis

1

1. Control Axes

1.1 Coordinate word and control axis

Function and purpose

In the standard specifications, there are 3 control axes. When using E68, up to 4 axes can be

controlled.

The designation of the processing direction responds to those axes and uses a coordinate word

made up of alphabet characters that have been decided beforehand.

Program coordinates

Direction o

f

table movement

Direction o

f

table movement

Bed

X-Y table

+Z

+Y

+X

+Y

Workpiece

X-

Y

table

P

rogram coor

di

nates

Direction o

f

table

movement

Di

rect

i

on o

f

ta

bl

e

revolution

+Z

+C

+X

+Y

+C

Workpiece

X-Y and revolving table [E68]

1. Control Axes

1.2 Coordinate systems and coordinate zero point symbols

2

1.2 Coordinate systems and coordinate zero point symbols

Function and purpose

: Reference point

: Machine coordinate zero point

: Work coordinate zero points (G54 - G59)

Basic machine coordinate s

y

stem

Machine

zero

p

oint

1st re

f

erence

point

Work coordinate

s

y

stem 3

(

G56

)

Work coordinate

system 2 (G55)

Work coordinate

s

y

stem 1

(

G54

)

Work coordinate

system 6 (G59)

Work coordinate

system 5 (G58)

Work

coordinate

system 4

(G57)

Local

coordinate

system

(G52)

-Y

y

3

-X

y

2

y

1

y

5

x

1

x

3

x

2

x

5

2. Input Command Units

2.1 Input command units

3

2. Input Command Units

2.1 Input command units

Function and purpose

These are the units used for the movement amounts in the program as commanded by the MDI

input and command tape. They are expressed in millimeters, inches or degrees (°).

2.2 Input setting units

Function and purpose

These are the units of setting data which are used, as with the compensation amounts, in common

for all axes.

The input setting units and input command units can be selected from the following types for each

axis with the parameters. (For further details on settings, refer to the Operation Manual.)

(1) When using E60

Linear axis

Input unit parameters

Millimeter Inch

Rotary axis (°)

Input command

unit

#1015 cunit = 10 0.001 0.0001 0.001

Input setting unit #1003 iunit = B 0.001 0.0001 0.001

(2) When using E68

Linear axis

Input unit parameters

Millimeter Inch

Rotary axis (°)

#1015 cunit = 10 0.001 0.0001 0.001 Input command

unit

#1015 cunit = 1 0.0001 0.00001 0.0001

#1003 iunit = B 0.001 0.0001 0.001

Input command

unit

#1003 iunit = C 0.0001 0.00001 0.0001

(Note 1) Inch/metric conversion is performed in either of 2 ways: conversion from the parameter

screen ("#1041 I_inch: valid only when the power is switched on) and conversion using

the G command (G20 or G21).

However, when a G command is used for the conversion, the conversion applies only to

the input command units and not to the input setting units.

Consequently, the tool offset amounts and other compensation amounts as well as the

variable data should be preset to correspond to inches or millimeters.

(Note 2) The millimeter and inch systems cannot be used together.

(Note 3) During circular interpolation on an axis where the input command units are different, the

center command (I, J, K) and the radius command (R) can be designated by the input

setting units. (Use a decimal point to avoid confusion.)

3. Data Formats

3.1 Tape codes

4

3. Data Formats

3.1 Tape codes

Function and purpose

The tape command codes used for this controller are combinations of alphabet letters (A, B, C, ...

Z), numbers (0, 1, 2 ... 9) and signs (+, -, / ...). These alphabet letters, numbers and signs are

referred to as characters. Each character is represented by a combination of 8 holes which may, or

may not, be present.

These combinations make up what is called codes.

This controller uses, the ISO code (R-840).

(Note 1) If a code not given in the tape code table in Fig. 1 is assigned during operation, program

error (P32) will result.

(Note 2) For the sake of convenience, a semicolon " ; " has been used in the CNC display to

indicate the end of a block (EOB/IF) which separates one block from another. Do not

use the semicolon key, however, in actual programming but use the keys in the

following table instead.

CAUTION

" ; ", "EOB", "%", and "EOR" are symbols used for explanation. The actual codes for ISO are

"CR, LF" ("LF") and "%".

The programs created on the Edit screen are stored in the NC memory in a "CR, LF" format,

however, the programs created with external devices such as the FLD or RS-232C may be

stored in an "LF" format.

The actual codes for EIA are "EOB (End of Block)" and "EOR (End of Record)".

Detailed description

EOB/EOR keys and displays

Code used

Key used

ISO Screen display

End of block LF or NL ;

End of record % %

(1) Significant data section (label skip function)

All data up to the first EOB ( ; ), after the power has been turned on or after operation has been

reset, are ignored during automatic operation based on tape, memory loading operation or

during a search operation. In other words, the significant data section of a tape extends from

the character or number code after the initial EOB ( ; ) code after resetting to the point where

the reset command is issued.

3. Data Formats

3.1 Tape codes

5

(2) Control out, control in

When the ISO code is used, all data between control out "(" and control in ")" are ignored,

although these data appear on the setting and display unit. Consequently, the command tape

name, number and other such data not directly related to control can be inserted in this

section.

This information (except (B) in the tape codes) will also be loaded, however, during tape

loading. The system is set to the "control in" mode when the power is witched on.

L C S L

F R

G

00X-85000Y-64000(CUTTE

R

P

RE T URN )

F

•

••

•

●

••

•

••

•

•••

•

•••

•

••

•

•••

•

••••

•

••••

•

••

•

•••

••

••••

••

•••

•

•••

••••

•

••

•

••

•••

••••

•

••••

••

•

••••

•

••

••••

••

•

Operator information print-out example

Information in this section is ignored and nothing is executed.

Example of ISO code

(3) EOR (%) code

Generally, the end-or-record code is punched at both ends of the tape. It has the following

functions:

(a) Rewind stop when rewinding tape (with tape handler)

(b) Rewind start during tape search (with tape handler)

(c) Completion of loading during tape loading into memory

(4) Tape preparation for tape operation (with tape handler)

Initial block

Last block

2m

10cm

%

2m

10cm %

(EOR)

(EOR)(EOB)

(EOB)

(EOB)(EOB)

;;;;

･････････

･････････････････････

If a tape handler is not used, there is no need for the 2-meter dummy at both ends of the tape

and for the head EOR (%) code.

3. Data Formats

3.1 Tape codes

6

8

7

6

5

4

3

2

1

Channel No.

•

1

•

2

•

••

3

•

4

•

• •

5

•

••

6

•

•••

7

•

••

•

8

•

••

•

9

•

0

•

A

•

B

••

•

••

C

•

D

••

•

• •

E

••

•

••

F

•

•••

G

• •

•

H

•• •

•

I

•• •

•

J

• •

•

••

K

•• •

•

L

• •

•

• •

M

• •

•

••

N

•• •

•

•••

O

• •

•

P

•• •

•

Q

•• •

•

R

• •

•

••

S

•• •

•

T

• •

•

• •

U

• •

•

••

V

•• •

•

•••

W

•• ••

•

X

• ••

•

Y

• ••

•

Z

•

••

+

•

• •

-

•

••

.

•

,

•

•••

/

•

• •

%

•

LF

(

Line Feed

)

or NL

•

(

Control Out

)

•

)

(

Control In

)

•

••

•

:

•

••

#

•

*

•

••

•

• •

=

•• ••

•

••

[

•• ••

•

• •

]

•

SP

(

Space

)

• •

•

• •

CR(Carriage Return)

• •

•

BS

(

Back S

p

ace

)

•

HT

(

Horizontal Tab

)

•

••

&

•

!

•

$

•

•••

’ (Apostrophe)

•

••

•

••

;

•

••

•

<

•

••

•

••

>

•

••

•

•••

?

••

•

@

•

”

••

•

••

•

•••

DEL

(

Delete

)

•

NULL

••

•

••

•

•••

DEL

(

Delete

)

•

• Under the ISO code, IF or NL is EOB and % is EOR.

• Under the ISO code, CR is meaningless, and EOB will not occur.

A

B

ISO code (R-840)

Feed holes

Code A are stored on tape but an error results (except when they are used in the comment

section) during operation.

The B codes are non-working codes and are always ignored. Parity V check is not executed.

Table of tape codes

3. Data Formats

3.2 Program formats

7

3.2 Program formats

Function and purpose

The prescribed arrangement used when assigning control information to the controller is known as

the program format, and the format used with this controller is called the "word address format".

Detailed description

(1) Word and address

A word is a collection of characters arranged in a specific sequence. This entity is used as the

unit for processing data and for causing the machine to execute specific operations. Each

word used for this controller consists of an alphabet letter and a number of several digits

(sometimes with a "-" sign placed at the head of the number.).

A

lphabet (address)

Word

Numerals

Word configuration

*

The alphabet letter at the head of the word is the address. It defines the meaning of the

numerical information which follows it.

For details of the types of words and the number of significant digits of words used for this

controller, refer to containing the "format details".

(2) Blocks

A block is a collection of words. It includes the information which is required for the machine to

execute specific operations. One block unit constitutes a complete command. The end of each

block is marked with an EOB (end-of-block) code.

(Example 1:)

G0X - 1000 ;

G1X - 2000F500 ;

(Example 2:)

(G0X - 1000 ; )

G1X - 2000F500 ;

(3) Programs

A program is a collection of several blocks.

2 blocks

Since the semicolon in the parentheses will not result

in an EOB

,

it is 1 block.

3. Data Formats

3.2 Program formats

8

Metric command Inch command

Rotary axis

(Metric command)

Rotary axis

(Inch command)

Program number 08

← ← ←

Sequence number N5

← ← ←

Preparatory function G3/G21

← ← ←

0.001(°) mm/

0.0001 inch

X+53 Y+53 Z+53 α+53 X+44 Y+44 Z+44 α+44 X+53 Y+53 Z+53 α+53 X+53 Y+53 Z+53 α+53

Movement

axis

0.0001(°) mm/

0.00001 inch

X+44 Y+44 Z+44 α+44 X+35 Y+35 Z+35 α+35 X+44 Y+44 Z+44 α+44 X+44 Y+44 Z+44 α+44

0.001(°) mm/

0.0001 inch

I+53 J+53 K+53 R+53 I+44 J+44 K+44 R+44 I+53 J+53 K+53 R+53

I+44 J+44 K+44 R+44

(Note 5)

Arc and

cutter

radius

0.0001(°) mm/

0.00001 inch

I+44 J+44 K+44 R+44 I+35 J+35 K+35 R+35 I+44 J+44 K+44 R+44

I+35 J+35 K+35 R+35

(Note 5)

0.001(°) mm/

0.0001 inch

F63(Feed per minute)

F43(Feed per revolution)

F44(Feed per minute)

F34(Feed per revolution)

F63(Feed per minute)

F43(Feed per revolution)

F44(Feed per minute)

F34(Feed per revolution)

(Note 6)Feed

function

0.0001 (°) mm/

0.00001 inch

F54(Feed per minute)

F34(Feed per revolution)

F35(Feed per minute)

F25(Feed per revolution)

F54(Feed per minute)

F34(Feed per revolution)

F35(Feed per minute)

F25(Feed per revolution)

(Note 6)

Dwell X+53/P+53 or X+53/P+8

← ← ←

Tool offset

H3 D3

← ← ←

Miscellaneous function (M)

M8

← ← ←

Spindle function (S)

S8

← ← ←

Tool function (T)

T8

← ← ←

2nd miscellaneous function A8/B8/C8

← ← ←

Subprogram

P8 H5 L4

← ← ←

0.001(°) mm/

0.0001 inch

R+53 Q53 P8 L4

← ← ←

Fixed

cycle

0.0001(°) mm/

0.00001 inch

R+44 Q44 P8 L4

← ← ←

[Format details]

(Note 1) α indicates the additional axis address, such as A, B or C.

(Note 2) The No. of digits check for a word is carried out with the maximum number of digits of that

address.

(Note 3) Numerals can be used without the leading zeros.

(Note 4) The meanings of the details are as follows :

Example 1 : 08 : 8-digit program number

Example 2 : G21 : Dimension G is 2 digits to the left of the decimal point, and 1 digit to the right.

Example 3 : X+53 : Dimension X uses + or - sign and represents 5 digits to the left of the

decimal point and 3 digits to the right.

For example, the case for when the X axis is positioned (G00) to the 45.123 mm position in the

absolute value (G90) mode is as follows :

G00

X45.123 ;

3 digits below the decimal point

5 digits above the decimal point, so it's +00045, but the leading zeros and the

mark (+) have been omitted.

G0 is possible.

(Note 5) If an arc is commanded using a rotary axis and linear axis while inch commands are being used,

the degrees will be converted into 0.1 inches for interpolation.

(Note 6) While inch commands are being used, the rotary axis speed will be in increments of 10 degrees.

Example: With the F1. (per-minute-feed) command, this will become the 10 degrees/minute

command.

(Note 7) The decimal places below the decimal point are ignored when a command, such as an S

command, with an invalid decimal point has been assigned with a decimal point.

3. Data Formats

3.2 Program formats

9

(Note 8) This format is the same for the value input from the memory, MDI or setting and display unit.

(Note 9) Command the program No. in an independent block. Command the program No. in the head

block of the program.

(Note 10) Minimum input setting unit "C" (0.0001 (°) mm/0.00001 inch) is a specification of the E68 system.

When using E60, the unit cannot be used.

3. Data Formats

3.3 Program address check function

10

3.3 Program address check function

Function and purpose

The program can be checked in word units when operating machining programs.

Detailed description

(1) Address check

This function enables simple checking of program addresses in word units. If the alphabetic

characters are continuous, the program error (P32) will occur. Availability of this function is

selected by the parameter "#1227 aux11/bit4".

Note that an error will not occur for the following:

(1) Reserved words

(2) Comment statements

(2) Word range check

When the operation expression is used for the word data, check whether one word data is

enclosed in brackets "[ ]" or not.

If it is not enclosed, the program error (P33) will occur.

Availability of this function is selected by the parameter "#1274 ext10/bit7".

Example of program

(1) Example of program for address check

(Example 1) When there are no numbers following an alphabetic character.

G28X; → An error will occur. Change to "G28 X0;", etc.

(Example 2) When a character string is illegal.

TEST; → An error will occur. Change to "(TEST);", etc.

(2) Example of program for word range check

An error (P33) will occur. Change as shown below.

X-100.-#24

Z+#500*TAN[#1]

Y-SIN[60.]

→

X-[100.+#24]

Z+[#500*TAN[#1]]

Y-SIN[60.]

The numbers of brackets that can be used for one word data are maximum five.

If six brackets or more are commanded, the program error (P280) will occur.

3. Data Formats

3.4 Tape memory format

11

3.4 Tape memory format

Function and purpose

(1) Storage tape and significant sections

The others are about from the current tape position to the EOB. Accordingly, under normal

conditions, operate the tape memory after resetting.

The significant codes listed in "Table of tape codes" in "3.1 Tape Codes" in the above

significant section are actually stored into the memory. All other codes are ignored and are not

stored.

The data between control out "(" and control in ")" are stored into the memory.

3.5 Optional block skip ; /

Function and purpose

This function selectively ignores specific blocks in a machining program which starts with the "/"

(slash) code.

Detailed description

(1) Provided that the optional block skip switch is ON, blocks starting with the "/" code are ignored.

They are executed if the switch is OFF.

Parity check is valid regardless of whether the optional block skip switch is ON or OFF.

When, for instance, all blocks are to be executed for one workpiece but specific block are not

to be executed for another workpiece, the same command tape can be used to machine

different parts by inserting the "/" code at the head of those specific blocks.

Precautions for using optional block skip

(1) Put the "/" code for optional block skip at the beginning of a block. If it is placed inside the block,

it is assumed as a user macro, a division instruction.

Example : N20 G1 X25./Y25. ;.....NG (User macro, a division instruction; a program error

results.)

/N20 G1 X25. Y25. ; ....OK

(2) Parity checks (H and V) are conducted regardless of the optional block skip switch position.

(3) The optional block skip is processed immediately before the pre-read buffer.

Consequently, it is not possible to skip up to the block which has been read into the pre-read

buffer.

(4) This function is valid even during a sequence number search.

(5) All blocks with the "/" code are also input and output during tape storing and tape output,

regardless of the position of the optional block skip switch.

3. Data Formats

3.6 Program/sequence/block numbers ; O, N

12

3.6 Program/sequence/block numbers ; O, N

Function and purpose

These numbers are used for monitoring the execution of the machining programs and for calling

both machining programs and specific stages in machining programs.

(1) Program numbers are classified by workpiece correspondence or by subprogram units, and

they are designated by the address "0" followed by a number with up to 8 digits.

(2) Sequence numbers are attached where appropriate to command blocks which configure

machining programs, and they are designated by the address "N" followed by a number with

up to 5 digits.

(3) Block numbers are automatically provided internally. They are preset to zero every time a

program number or sequence number is read, and they are counted up one at a time unless

program numbers or sequence numbers are commanded in blocks which are subsequently

read.

Consequently, all the blocks of the machining programs given in the table below can be

determined without further consideration by combinations of program numbers, sequence

numbers and block numbers.

Monitor display

Machining program

Program No. Sequence No. Block No.

O12345678 (DEMO, PROG) ; 12345678 0 0

G92 X0 Y0 ; 12345678 0 1

G90 G51 X-150. P0.75 ; 12345678 0 2

N100 G00 X-50. Y-25. ; 12345678 100 0

N110 G01 X250. F300 ; 12345678 110 0

Y-225. ; 12345678 110 1

X-50. ; 12345678 110 2

Y-25.; 12345678 110 3

N120 G51 Y-125. P0.5 ; 12345678 120 0

N130 G00 X-100. Y-75. ; 12345678 130 0

N140 G01 X-200. ; 12345678 140 0

Y-175. ; 12345678 140 1

X-100. ; 12345678 140 2

Y-75. ; 12345678 140 3

N150 G00 G50 X0 Y0 ; 12345678 150 0

N160 M02 ; 12345678 160 0

%

Page is loading ...

Mitsubishi Electric EZ Motion E60/E68 Series Programming Manual

Mitsubishi Electric EZ Motion E60/E68 Series Programming Manual

Related papers

Other documents